acceptable converging?
 

Hello,

My teacher said that to accomplish a good analysis, I should have a converging of 10^-6 for x,y,z velocities and energy. Is this true? I have a high quality structured mesh but could not reach that converging. The residuals are as shown. The results are sensible. Might these residuals be valid ?

Your teacher is wrong. Residuals are indicative, but not conclusive. They provide a relative level of change. How far your residuals will pratically reduce depends on the geometry, on the parameter of interest, on the goodness of the initial guess, etcetera. I've seen cases where all residuals were 10^-3 and the problem was converged, and situations where all were 10^-6 but still the situation was significantly changing over the iterations. So, residuals indicate whether your solution is getting better or worse, but in themselves should not be used to judge convergence on.

Better is to judge some physical parameters. For example, does the average velocity in the domain reach a constant value over the iterations. Does the average temperature (if you consider energy)? Does the torque of an impeller reach a steady value, etc., etc. Depending on the problem, you may tune your choice of indicators. For example, are you interested in a surface nusselt number, then check if this reaches a steady value over the iterations. What is good enough depends on your own preference, and on the situation. Typically, I'm satisfied when the parameter of interest stays within a 0.01% range over 1000 iterations, but it may depend on the situation.

Havind said that, I have seen no situations where such parameters were sufficiently constant while the residuals were still around 10^-2. So although I can't say with certainty, I'd be surprised if your simulation was sufficiently converged here.

Thank you for clarifying. But I cant understand why these residuals are going up and down steadily as seen. They never get a decisivness. So I cant get rid of my doubts.

Could you kindly explain how to check a physical parameter over iterations in order for me to look at it the way you suggested. Im sorry Im limited in fluent. Thanks a lot.

go to 'volume integrals', select the parameter you want to follow (i.e. velocity magnitude, x-vel, etc..) and click 'plot'. The value then will be tracked over the iterations, just like residuals. Also, you can export it to a text file (select write and add a path), so you can check whether or not any oscillations in the value are significant (although quite frequently this is obvious from the direct plot)

Thanks a lot again, it looks as a reasonable approach and hope the parameters of interest stay constant after some iterations.

Hi,

Unfortunately I cant reach a stability. What might be a possible factor? May the residual attached stay constant after more iterations ?

Mesh quality can always be a problem; what did you mean with good quality mesh? Also, it may help to change your under-relaxation factors under solution controls. If you are making too big steps (too high factors) you may keep oscillating around a better solution without being able to reach it. Especially continuity tends to be quite sensitive, try reducing the under-relaxation for continuity to 0.1 or 0.2.

You could choose to use lower order discretization schemes too, but these of course provide additional stability at the cost of extra diffusion.

Ceesh,

Thank you for your interest. Could you look over the thread in the following link if you are able to make time any time. It lays the problem out clearly I guess.

http://www.cfd-online.com/Forums/flu...residuals.html

min orthogonal guality is about 0.9 and aspect ratio is about 70